要在原理图中放置符号，请使用 按钮或A 快捷键。此时将出现“选择符号”对话框，您可以在其中选择要添加的符号。符号按符号库分组。

To place a symbol in your schematic, use the button or the A hotkey. The Choose Symbols dialog appears and lets you select a symbol to add. Symbols are grouped by symbol library.

默认情况下，仅显示符号/库名称和描述列。右键单击列标题并选择“选择列”即可添加其他列。

By default, only the symbol/library name and description columns are shown. Additional columns can be added by right-clicking the column header and selecting Select Columns.

“选择符号”对话框会根据您在搜索框中输入的内容，按名称、关键字、描述以及所有其他符号字段筛选符号。您可以点击按钮选择按字母顺序或按最佳匹配度对搜索结果进行排序。

The Choose Symbol dialog filters symbols by name, keywords, description, and all additional symbol fields according to what you type into the search field. You can choose to sort search results alphabetically or by best match by clicking on the button.

提供一些高级筛选器：

Some advanced filters are available:

如果符号指定了默认封装，则会在右下角预览该封装。如果符号包含封装筛选器，则可以在右侧的封装下拉菜单中选择符合筛选条件的备选封装。

If the symbol specifies a default footprint, this footprint will be previewed in the lower right. If the symbol includes footprint filters, alternate footprints that satisfy the footprint filters can be selected in the footprint dropdown menu at right.

选择要放置的符号后，该符号将附加到光标上。在原理图中左键单击所需位置即可将符号放置到原理图中。在将符号放置到原理图之前，您可以使用快捷键或右键单击上下文菜单旋转、镜像符号并编辑其字段。这些操作也可以在放置后执行。

After selecting a symbol to place, the symbol will be attached to the cursor. Left clicking the desired location in the schematic places the symbol into the schematic. Before placing the symbol in the schematic, you can rotate it, mirror it, and edit its fields, by either using the hotkeys or the right-click context menu. These actions can also be performed after placement.

如果选中“放置重复副本”选项，KiCad 在放置一个符号后会开始放置该符号的另一个副本。此过程会一直持续到用户按下停止键为止Esc。

If the Place repeated copies option is checked, after placing a symbol KiCad will start placing another copy of the symbol. This process continues until the user presses Esc.

对于包含多个单位的符号，如果选中“放置所有单位”选项，KiCad 在放置符号后将开始放置下一个单位。此过程将持续到放置完最后一个单位或用户按下 Esc.

For symbols with multiple units, if the Place all units option is checked, after placing the symbol KiCad will start placing the next unit in the symbol. This continues until the last unit has been placed or the user presses Esc.

电源符号是代表与电源网络连接的符号。这些符号已分组存储在power符号库中，因此可以使用符号选择器进行放置。然而，由于电源放置操作频繁，因此也提供了一个 工具。该工具与符号选择器类似，区别在于它直接在符号库以及任何其他包含电源符号的符号库中进行搜索。power

A power symbol is a symbol representing a connection to a power net. The symbols are grouped in the power library, so they can be placed using the symbol chooser. However, as power placements are frequent, the tool is available. This tool is similar, except that the search is done directly in the power library and any other library that contains power symbols.

可以使用移动 ( M) 或拖动 ( G) 工具移动符号。这些工具作用于选定的符号；如果没有选择任何符号，则作用于光标下的符号。

Symbols can be moved using the Move (M) or Drag (G) tools. These tools act on the selected symbol, or if no symbol is selected they act on the symbol under the cursor.

移动工具会移动符号本身，而不会保持与符号引脚的有线连接。

The Move tool moves the symbol itself without maintaining wired connections to the symbol pins.

拖动工具可以移动符号，而不会断开与引脚的有线连接，因此也会移动连接的导线。

The Drag tool moves the symbol without breaking wired connections to its pins, and therefore moves the connected wires as well.

您还可以通过点击并拖动鼠标来拖动符号，具体取决于“首选项”中的“鼠标和触摸板”部分的“左键拖动手势”设置 。

You can also Drag symbols by clicking and dragging them with the mouse, depending on the Left button drag gesture setting in the Mouse and Touchpad section of Preferences.

R符号还可以沿 X ( X) 或 Y ( ) 方向旋转 ( ) 或镜像Y。

Symbols can also be rotated (R) or mirrored in the X (X) or Y (Y) directions.

原理图中的符号可以单独编辑，包括其属性（字段、特性等）、引脚和图形。编辑原理图中的符号只会影响该符号的特定实例；不会影响原理图中该符号的任何其他副本，也不会影响库符号。

Symbols in the schematic can be individually edited, both in terms of their properties (fields, attributes, etc.) and in terms of their pins and graphics. Editing a symbol in the schematic only affects that particular instance of the symbol; it does not affect any other copies of that symbol in the schematic, and it does not affect the library symbol.

要编辑原理图中符号的属性，请打开其属性对话框（E）。您也可以双击该符号。

To edit the properties of a symbol in the schematic, open its properties dialog (E). You can also double-click the symbol.

“符号属性”窗口以表格形式显示符号的所有字段。您可以添加新字段，也可以删除、编辑、重新排序、移动或调整现有字段的大小。字段可以任意命名，但以 `_` 开头的名称（ ki_例如 ` _`）已被 KiCad 保留，不应用于用户自定义字段。当从原理图更新 PCBki_description时，所有符号字段都将添加到符号对应的封装中。

The Symbol Properties window displays all the fields of a symbol in a table. New fields can be added, and existing fields can be deleted, edited, reordered, moved, or resized. Fields can be arbitrarily named, but names beginning with ki_, e.g. ki_description, are reserved by KiCad and should not be used for user fields. All symbol fields will be added to the symbol’s corresponding footprint when the PCB is updated from the schematic.

每个字段的名称和值都可以显示或隐藏，并且有多种格式设置选项：水平和垂直对齐方式、方向、位置、字体、文本颜色、文本大小以及粗体/斜体。还可以为每个字段启用自动定位功能。对于正常显示的符号（不旋转或镜像），其显示位置始终相对于符号的锚点。

Each field’s name and value can be visible or hidden, and there are several formatting options: horizontal and vertical alignment, orientation, position, font, text color, text size, and bold/italic emphasis. Field autoplacement can also be enabled on a per-field basis. The displayed position is always indicated for a normally displayed symbol (no rotation or mirroring) and is relative to the anchor point of the symbol.

某些字段具有特殊行为：

Several fields have special behavior:

符号具有多个属性，这些属性会影响 KiCad 其他部分对符号的处理方式。

Symbols have several attributes that affect how the symbols are treated by other parts of KiCad.

要编辑符号的形式，例如其引脚和图形，您需要使用符号编辑器。编辑器中有两个按钮用于打开符号，具体取决于您要编辑原理图中符号的单个副本，还是库中符号的源副本。

To edit the symbols’s form, i.e. its pins and graphics, you need to use the symbol editor. There are two buttons for opening a symbol in the editor, depending on whether you want to edit a single copy of a symbol in the schematic or a symbol’s source copy in the library.

“从库更新符号…”按钮用于将原理图中的符号副本更新为与库中的副本一致。“更改符号…” 按钮用于将当前符号替换为库中的另一个符号。这些功能将 在后面详细介绍。

The Update Symbol from Library…​ button is used to update the schematic’s copy of the symbol to match the copy in the library. The Change Symbol…​ button is used to swap the current symbol to a different symbol in the library. These functions are described later.

“仿真模型…”按钮打开 仿真模型编辑器，用于指定符号在SPICE 仿真中的行为。

The Simulation Model…​ button opens the Simulation Model Editor for specifying the symbol’s behavior in SPICE simulations.

符号引脚可以定义备用引脚功能。备用引脚功能允许您在原理图中放置符号时，为引脚选择不同的名称、电气类型和图形样式。这可用于具有多种功能的引脚，例如微控制器引脚。

Symbol pins can have alternate pin functions defined for them. Alternate pin functions allow you to select a different name, electrical type, and graphical style for a pin when a symbol has been placed in the schematic. This can be used for pins that have multiple functions, such as microcontroller pins.

在原理图中放置符号后，即可选择备用引脚功能。引脚功能在 “符号属性”对话框的“引脚功能”选项卡中选择。备用定义可在“备用分配”列的下拉列表中选择。您也可以右键单击引脚，然后从“引脚功能”菜单中选择新的功能来选择备用引脚。

Alternate pin functions are selected once a symbol has been placed in the schematic. The pin function is selected in the Pin Functions tab of the Symbol Properties dialog. Alternate definitions are selectable in the dropdown in the Alternate Assignment column. You can also select an alternate pin by right-clicking the pin and selecting a new function from the Pin Function menu.

如果某个引脚具有其他功能，则引脚名称旁边会显示一个小型图形指示器，如下图所示。要全局显示或隐藏这些指示器，请使用“视图” → “显示引脚备用图标”。

Pins that have alternate functions available are displayed with a small graphical indicator next to the pin name, as shown in the screenshot below. To globally show or hide these indicators, use View → Show Pin Alternate Icons.

有关如何向符号添加备用引脚功能的信息，请参阅符号编辑器文档。

For information on how to add alternate pin functions to symbols, see the symbol editor documentation.

当向原理图添加符号时，KiCad 会将库符号的副本嵌入到原理图中，从而使原理图独立于系统库。已添加到原理图中的符号不​​会在库更改时自动更新。库符号的更改需要手动同步到原理图，以避免原理图发生意外更改。

When a symbol is added to the schematic, KiCad embeds a copy of the library symbol in the schematic so that the schematic is independent of the system libraries. Symbols that have been added to the schematic are not automatically updated when the library changes. Library symbol changes are manually synced to the schematic so that the schematic does not change unexpectedly.

要更新原理图中的符号以匹配相应的库符号，请使用“工具” → “从库更新符号…”选项，或者右键单击符号并选择“更新符号…”选项。您也可以从符号属性对话框访问此工具 。

To update symbols in the schematic to match the corresponding library symbol, use Tools → Update Symbols from Library…​, or right click a symbol and select Update Symbol…​. You can also access the tool from the symbol properties dialog.

对话框顶部有选项，可以选择要更新哪些符号：

The top of the dialog has options to choose which symbols will be updated:

对话框中间部分提供了一些选项，用于控制要更新符号的哪些部分。在左侧，您可以选择要修改（更新或重置）的字段。在右侧，您可以选择如何更新这些字段：

The middle of the dialog has options to control what parts of the symbol will be updated. On the left, you can select which fields will be modified (updated or reset). On the right, you can select how to update those fields:

对话框底部显示描述已执行的更新操作的消息，并提供筛选器以显示消息类型（错误、警告、操作和/或信息）。

The bottom of the dialog displays messages describing the update actions that have been performed, with filters for which types of messages to display (errors, warnings, actions, and/or infos).

要将现有符号更改为其他符号，请使用“编辑” → “更改符号…”选项，或者右键单击现有符号并选择 “更改符号…”选项。也可以从符号属性对话框访问此对话框 。

To change an existing symbol to a different symbol, use Edit → Change Symbols…​, or right click an existing symbol and select Change Symbol…​. This dialog is also accessible from the symbol properties dialog.

“更改符号”对话框的选项与“从库更新符号”对话框的选项非常相似。

The options for the Change Symbols dialog are very similar to the Update Symbols from Library dialog.

另一种将现有符号替换为新符号的方法是使用“工具” → “编辑符号库链接…”。此对话框包含一个表格，其中列出了设计中的每个符号，并按当前库符号分组。通过在“新库引用”列中选择新符号，您可以将现有符号的所有实例都指向新符号。如果 使用“从新库更新符号字段”选项，则现有符号的字段内容将更新为与新符号的字段内容匹配。

Another way to swap existing symbols for new ones is to use Tools → Edit Symbol Library Links…​. This dialog contains a table of every symbol in the design, grouped by current library symbol. By choosing a new symbol in the New Library Reference column, you can make all instances of the existing symbol instead point to the new symbol. If the Update symbol fields from new library option is used, the contents of the existing symbols' fields will be updated to match the new symbols' fields.

“映射孤立符号”按钮会尝试自动将孤立符号重新映射到活动库中同名的符号。例如，如果存在一个具有当前库引用的符号mylib:symbol123，但mylib找不到该库，“映射孤立符号”按钮将尝试在任何已存在的库中查找名为该符号的符号 symbol123。仅当原理图中存在孤立符号时，此按钮才可用（请参阅 旧版原理图部分）。

The Map Orphans button attempts to automatically remap orphaned symbols to symbols with the same name in an active library. For example, if there is a symbol with the current library reference mylib:symbol123, but the mylib library cannot be found, the Map Orphans button will attempt to find a symbol named symbol123 in any of the libraries that are present. This button is only enabled if orphaned symbols are present in the schematic (see the legacy schematics section).

此对话框主要用于管理出现在多个库中的符号，以便在不同库之间切换时使用。例如，如果原理图使用的符号同时存在于全局库和项目特定库中，则可以使用“符号库引用”对话框在全局符号和等效的项目特定符号之间切换。它不具备对字段更新方式进行精细控制的功能；如需进行此类控制，请使用“更改符号”对话框。

This dialog is primarily useful for managing symbols that appear in multiple libraries, when you want to switch from one library to another. For example, if a schematic uses symbols that are in both a global library and a project-specific library, the Symbol Library References dialog could be used to switch between using the global symbols or the equivalent project-specific symbols. It does not have features for fine-grained control of how fields are updated; for that, use the Change Symbols dialog.

当原理图中的符号与原始符号库中的对应符号不一致时，可以使用“比较符号与库”工具来检查两个版本符号之间的差异。运行该工具的方法是：检查→比较符号与库。

When a symbol in a schematic diverges from the corresponding symbol in the original symbol library, you can use the Compare Symbol with Library tool to inspect the differences between the two versions of the symbol. Run the tool using Inspect → Compare Symbol With Library.

摘要选项卡显示符号的名称，包括其库和原理图参考标识符，并列出符号的原理图版本和库版本之间的差异。

The Summary tab shows the name of the symbol, including its library and schematic reference designator, and provides a list of the differences between the schematic and library versions of the symbol.

“可视化”选项卡以可视化的方式对比了原理图版本和库版本中的符号。它可以作为可视化差异比较工具使用。

The Visual tab shows a visual comparison of the schematic and library versions of the symbol. This can be used as a visual diff tool.

默认情况下，比较视图会将符号的两个版本叠加显示。为了更清晰地查看变化，您可以拖动选项卡底部的滑块，向右突出显示叠加视图中的库版本符号（使原理图版本符号更加透明），或向左突出显示原理图版本符号（使库版本符号更加透明）。滑块拖动到最右侧和最左侧时，原理图版本符号和库版本符号分别完全隐藏。来回拖动滑块有助于更清晰地查看变化。

By default, the comparison displays both versions of the symbol superimposed on each other. To see the changes more easily, you can drag the slider at the bottom of the tab to the right to emphasize the library version of the symbol in the superimposed view (making the schematic version of the symbol more transparent) or drag it to the left to emphasize the schematic version (making the library version more transparent). At the far right and left ends of the slider, the schematic and library versions of the symbol, respectively, are fully hidden. It may be helpful to drag the slider back and forth to see the changes more clearly.

您可以按下A/B按钮或使用/热键，快速在原理图版本和库版本之间切换。

You can press the A/B button, or use the / hotkey, to quickly toggle back and forth between the schematic and library versions.

上面的截图显示了符号与原理图版本的视觉对比（已弱化处理）。可以看到，原理图中部分透明的引脚 5 与库符号中完全不透明的引脚 5 位置不同。这表明该引脚在原理图或库符号中的位置发生了变化。

The screenshot above shows a visual comparison with the schematic version of the symbol deemphasized. You can see a partially transparent pin 5 (from the schematic version of the symbol) is in a different location than the fully opaque pin 5 (from the library symbol). This indicates that the pin was moved in either the schematic or library version of the symbol.

符号字段表允许您在电子表格界面中查看和修改所有符号的字段值。您可以使用按钮打开符号字段表。

The Symbol Fields Table allows you to view and modify field values for all symbols in a spreadsheet interface. You can open the Symbol Fields Table with the button.

使用方向键可以在单元格中导航，或者使用Tab/ Shift+Tab分别向右/向左和Enter向下移动。

Cells are navigated with the arrow keys, or with Tab / Shift+Tab to move right / left and Enter to move down, respectively.

Ctrl您可以通过点击并拖动来选择一系列单元格。复制 ( +C ) 或粘贴操作会将整个选定的单元格区域复制到 ( Ctrl+V ) 指定位置。从表格中复制一系列单元格对于创建物料清单 (BOM) 非常有用。有关复制和粘贴单元格的更多详细信息，请参见下文。

A range of cells can be selected by clicking and dragging. The whole range of selected cells will be copied (Ctrl+C) or pasted into (Ctrl+V) on a copy or paste action. Copying a range of cells from the table can be useful for creating a BOM. More details of copying and pasting cells are described below.

左侧窗格包含所有可用符号字段的列表，以及一些 虚拟字段，例如“数量”和“项目编号”。您可以使用“ 显示”复选框在主表中添加或删除任何符号字段（也可以通过右键单击主表标题来显示或隐藏字段）。可以使用 按钮添加新的符号字段；该名称的字段将添加到每个符号中。要重命名字段（这将更改所有符号中的字段名称），请使用 按钮。按钮会从所有符号中删除该字段。

The left pane contains a list of all available symbol fields, as well as some virtual fields such as Quantity and Item Number. You can add or remove any symbol field from the main table on using the Show checkboxes (fields can also be shown or hidden by right-clicking on the header of the main table). New symbol fields can be added using the button; a field with that name will be added to every symbol. To rename the field, which changes the field name in all symbols, use the button. The button deletes the field from all symbols.

每个字段都有自己的列标签，该标签显示在符号字段表和导出的物料清单 (BOM) 中对应列的顶部。每个字段的列标签显示在左侧窗格的第二列中。列标签不必与字段名称相同。要更改字段的列标签，请在左侧窗格中选择该字段所在的行，然后再次单击该行的列标签单元格进行编辑。

Each field has its own column label, which is displayed at the top of the corresponding column in the symbol fields table and in exported BOMs. The column label for each field is shown in the second column of in the left pane. A column label does not have to match the field name. To change a field’s column label, select the field’s row in the left pane, then click again in the column label cell of that row to edit it.

可以使用“分组依据”复选框，按任意符号字段对相似的符号进行分组。如果所有符号的“分组依据”字段都相同，则这些符号将被分组到表格中的同一行。单击行左侧的箭头，即可展开分组行以显示各个符号。“符号分组”复选框用于启用或禁用符号分组，“分组 依据”按钮用于重新计算分组。

Similar symbols can optionally be grouped by any symbol field using the Group By checkboxes. Symbols are grouped into a single row in the table if all of their Group By fields are identical. The grouped row can be expanded to show the individual symbols by clicking the arrow at the left of the row. The Group Symbols checkbox enables or disables symbol grouping, and the button recalculates groupings.

预设可用于配置字段列表。预设会存储要显示的字段、用于分组的字段以及列顺序。您可以创建并保存自己的预设，也可以使用几个默认预设之一。自定义预设可以在此对话框或 “原理图设置”对话框中删除。

Presets are available to configure the list of fields. Presets store which fields are displayed, which fields are used for grouping, and the column order. You can create and save your own presets or use one of several default presets. Custom presets can be deleted in this dialog or in the Schematic Setup dialog.

您可以使用顶部的“筛选”文本框按参考标识符筛选符号。筛选器支持通配符：*可匹配任意数量的任意字符（包括零个字符），也?可匹配任意单个字符。您还可以更改显示范围，仅显示当前图纸中的符号、当前图纸及其所有子图纸中的符号，或显示整个项目中的符号。选中“排除 DNP”复选框，即可选择性地排除设置了 DNP（不填充）属性的符号。

Symbols can be filtered by reference designator using the Filter textbox at the top. The filter supports wildcards: * matches any number of any characters, including none, and ? matches any single character. You can also change the display scope, showing only symbols in the current sheet, the current sheet and all of its subsheets, or the entire project. Symbols with the DNP (do not populate) attribute set can be optionally excluded by checking the Exclude DNP box.

您可以在此对话框中通过选择表格中的一行来进行交叉探测。根据对话框底部的“交叉探测操作”设置，此操作可以高亮显示原理图中的相应符号、选中原理图中的相应符号，或者不执行任何操作。根据 PCB 编辑器交叉探测设置，选择操作还可以选中电路板编辑器中符号的封装。

You can cross-probe from this dialog by selecting a row in the table. Depending on the Cross-probe action setting at the bottom of the dialog, this can highlight the corresponding symbol in the schematic, select the corresponding symbol in the schematic, or do nothing. The selection action can also select the symbol’s footprint in the board editor, depending on the PCB Editor cross-probing settings.

符号字段表也是一个物料清单工具。您可以使用 “导出”按钮将符号字段保存到外部文件。导出到物料清单的字段将与当前在电子表格视图中的显示完全一致。文件格式设置在“导出”选项卡中配置。有关导出物料清单的更多信息，请参阅物料清单工具文档。

The Symbol Fields Table is also a bill of materials tool. You can use the Export button to save the symbol fields to an external file. The fields are exported to the BOM exactly as they are currently shown in the spreadsheet view. File format settings are configured in the Export tab. For more information about exporting a BOM, see the BOM tool documentation.

启用自动注释后，添加到原理图中的符号将自动添加注释。您可以 在“原理图编辑器” → “注释选项”面板的“首选项”中选中“自动注释符号”复选框来启用自动注释。您也可以使用左侧工具栏中的按钮切换自动注释的启用/禁用状态。

When auto-annotation is enabled, symbols will be automatically annotated when they are added to the schematic. You can enable auto-annotation by checking the Automatically annotate symbols checkbox in the Schematic Editor → Annotation Options pane in Preferences. Auto-annotation can also be toggled using the button in the left toolbar.

当同时添加多个符号时，它们会根据“顺序”设置进行注释，按 X 或 Y 位置排序。

When multiple symbols are added simultaneously, they are annotated according to the Order setting, sorted by either X or Y position.

“编号”选项用于设置新参考编号的起始编号。该编号可以是可用的最小编号，也可以是基于图纸编号的编号。

The Numbering option sets the starting number for new reference designators. This can be the lowest available number, or a number based on the sheet number.

有关标注选项的更多信息，请参阅标注工具的文档 。

For more information about annotation options, see the documentation for the Annotation tool.

注释工具会自动为原理图中的符号分配参考标识符。要启动注释工具，请单击 顶部工具栏中的按钮。

The Annotation tool automatically assigns reference designators to symbols in the schematic. To launch the Annotation tool, click the button in the top toolbar.

该工具提供了多种选项来控制符号的注释方式。

The tool provides several options to control how symbols are annotated.

范围：选择注释是应用于整个原理图、仅应用于当前图纸，还是仅应用于选定的符号。如果 选中“递归到子图纸”选项，则会对所选范围内的子图纸中的符号重新添加注释；否则，子图纸中的符号将不会被重新添加注释。例如，如果选中“递归到子图纸”和“仅选择” ，则会对任何选定子图纸中的符号重新添加注释。

Scope: Selects whether annotation is applied to the entire schematic, to only the current sheet, or to only the selected symbols. If the Recurse into subsheets option is selected, symbols in subsheets of the selected scope will be reannotated; otherwise symbols in subsheets will not be reannotated. For example, if Recurse into subsheets and Selection only selected, symbols in any selected subsheets will be reannotated.

选项：选择注释是否应应用于所有符号并重置现有参考指示符，或者仅应用于未注释的符号。

Options: Selects whether annotation should apply to all symbols and reset existing reference designators, or apply only to unannotated symbols.

顺序： 选择编号方向。如果符号按 X 轴位置排序，则原理图左侧的所有符号编号都小于右侧的符号编号。如果符号按 Y 轴位置排序，则原理图顶部的所有符号编号都小于底部的符号编号。

Order: Chooses the direction of numbering. If symbols are sorted by X position, all symbols on the left side of a schematic sheet will be lower numbered than symbols on the right side of the sheet. If symbols are sorted by Y position, all symbols on the top of a sheet will be lower numbered than symbols at the bottom of the sheet.

编号：选择参考标识符编号的起始点。每个参考标识符都选取起始点以上未使用的最小数字。起始点可以是任意数字（通常为零），也可以是图纸编号乘以 100 或 1000，以便每个元件的参考标识符与其所在的原理图页相对应。

Numbering: Selects the starting point for numbering reference designators. The lowest unused number above the starting point is picked for each reference designator. The starting point can be an arbitrary number (typically zero), or it can be the sheet number multiplied by 100 or 1000 so that each part’s reference designator corresponds to the schematic page it is on.

清除注释按钮会清除所选范围内的所有参考标识符。

The Clear Annotation button clears all reference designators in the selected scope.

可以使用底部的复选框筛选注释消息，或使用“保存…”按钮将注释消息保存到报告中。

Annotation messages can be filtered with the checkboxes at the bottom or saved to a report using the Save…​ button.

导线用于直接在两点之间建立电气连接。要建立连接，一段导线的末端必须与另一段导线或引脚连接。只有导线的末端才能形成连接；如果一根导线穿过另一根导线的中间，则无法建立连接。

Wires are used to directly establish electrical connections between two points. To establish a connection, a segment of wire must be connected by its end to another segment or to a pin. Only wire ends create connections; if a wire crosses the middle of another wire, a connection will not be made.

未连接的导线末端会显示一个小方块，指示连接点。连接导线末端后，方块会消失。未连接的引脚会显示一个圆圈，连接后圆圈也会消失。

Unconnected wire ends have a small square that indicates the connection point. The square disappears when a connection is made to the wire end. Unconnected pins have a circle, which also disappears when a connection is made.

标签用于为导线和引脚分配网络名称。具有相同网络名称的导线被视为已连接，因此可以使用标签来建立连接，而无需绘制直接的导线连接线。

Labels are used to assign net names to wires and pins. Wires with the same net name are considered to be connected, so labels can be used to make connections without drawing direct wire connections.

一个网络只能有一个名称。如果同一个网络使用了两个不同的名称，则会违反 ERC 规则。网络列表中只会使用其中一个网络名称。最终的网络名称根据 以下规则确定。

A net can only have one name. If two different labels are placed on the same net, an ERC violation will be generated. Only one of the net names will be used in the netlist. The final net name is determined according to the rules described below.

标签有三种类型，每种类型的连接范围都不同。

There are three types of labels, each with a different connection scope.

总线是一种在原理图中将相关信号分组以简化复杂设计的手段。总线可以使用总线工具像绘制导线一样绘制，并像信号导线一样使用标签命名。

Buses are a way to group related signals in the schematic in order to simplify complicated designs. Buses can be drawn like wires using the bus tool , and are named using labels the same way signal wires are.

在下图所示的示意图中，许多引脚连接到总线，总线是中间的粗蓝线。

In the following schematic, many pins are connected to buses, which are the thick blue lines in the center.

电源符号是通常用于表示与电源网络连接的符号，例如VCC或GND。电源符号是虚拟的：它们并不代表 PCB 上的物理元件。

Power symbols are symbols that are conventionally used to represent a connection to a power net, such as VCC or GND. Power symbols are virtual: they do not represent a physical component on the PCB.

除了作为连接网络为电源轨的视觉指示外，电源符号还用于建立全局连接：两个电源符号可以Value 在原理图中的任意位置相互连接，不受图纸限制。电源符号的Value字段决定了所连接网络的名称。

In addition to being a visual indicator that the attached net is a power rail, power symbols make global connections: two power symbols with the Value connect to each other anywhere in the schematic, regardless of sheet. The power symbol’s Value field determines the name of the attached net.

在下图中，电源符号用于将电容器的正负极分别连接到VCC和GND网络。

In the figure below, power symbols are used to connect the positive and negative terminals of the capacitors to the VCC and GND nets, respectively.

KiCad 标准库中包含电源符号power，但也可以在任何库中创建电源符号。自定义电源符号的创建方法请参阅符号编辑器文档。除了创建新符号外，您还可以修改原理图中现有的电源符号：更改其Value字段将更改电源符号连接的网络。

In the KiCad standard library, power symbols are found in the power library, but power symbols can be created in any library. Creating custom power symbols is described in the symbol editor documentation. Instead of making a new symbol, you can also modify an existing power symbol in the schematic: changing its Value field will change the net the power symbol connects to.

原理图中的每个网络都被赋予一个名称，无论该名称是由用户指定还是由 KiCad 自动生成。

Every net in the schematic is assigned a name, whether that name is specified by the user or automatically generated by KiCad.

当多个标签附加到同一网络上时，最终的网络名称按以下优先级顺序确定：

When multiple labels are attached to the same net, the final net name is determined in the following order, from highest priority to lowest:

如果一张网上贴有多个相同类型的标签，则按字母顺序排列名称，并使用第一个标签。

If there are multiple labels of one type attached to a net, the names are sorted alphabetically and the first is used.

如果一张网状结构穿过 层级结构的多个层级，它将以层级结构中最高层级的名称命名，该层级必须具有层级标签或本地标签。通常情况下，本地标签的优先级高于层级标签。

If a net travels through multiple sheets of a hierarchy, it will take its name from the highest level of the hierarchy where it has a hierarchical label or local label. As usual, local labels take priority over hierarchical labels.

如果以上任何标签类型都没有连接到网络，则根据连接的符号引脚自动生成网络名称。

If none of the label types above are attached to a net, the net’s name is automatically generated based on the connected symbol pins.

PWR_FLAG上图中可以看到两个符号。它们向ERC表明这两个电源网络实际上VCC已GND连接到电源，因为这两个网络都没有直接连接电压调节器输出等电源。

Two PWR_FLAG symbols are visible in the screenshot above. They indicate to ERC that the two power nets VCC and GND are actually connected to a power source, as there is no explicit power source such as a voltage regulator output attached to either net.

如果没有这两个标志，ERC 工具将诊断为：错误：输入电源引脚未被任何输出电源引脚驱动。

Without these two flags, the ERC tool would diagnose: Error: Input Power pin not driven by any Output Power pins.

该PWR_FLAG符号可在符号库中找到power。将任意电源输出引脚连接到该网络即可达到相同效果。

The PWR_FLAG symbol is found in the power symbol library. The same effect can be achieved by connecting any power output pin to the net.

无连接标志（）用于指示引脚有意未连接。这些标志可以防止对有意未连接的引脚发出“未连接引脚”的 ERC 警告。此外，虽然堆叠在一起的符号引脚通常连接到同一网络，但如果为堆叠的引脚添加无连接标志，它们将连接到不同的网络。

No-connection flags () are used to indicate that a pin is intentionally unconnected. These flags prevent "unconnected pin" ERC warnings for pins that are intentionally unconnected. Also, while symbol pins that are stacked on top of each other are normally connected to the same net, if a no-connection flag is added to the stacked pins they will instead be connected to separate nets.

请注意，无连接标志与“未连接”符号引脚类型不同 ，尽管它们都能防止在相关引脚上出现“未连接引脚”ERC 警告，并防止堆叠引脚相互连接。

Note that no-connection flags are distinct from the "unconnected" symbol pin type, although they both prevent "unconnected pin" ERC warnings on the pin in question and prevent stacked pins from connecting to each other.

当符号的电源引脚可见时，必须像连接其他信号一样进行连接。然而，有时符号会绘制隐藏的电源输入引脚，这些引脚默认是隐式连接的。KiCad 会自动将类型为“电源输入”的不可见引脚连接到与其同名的全局网络。例如，如果一个符号有一个名为 `<power_input_pin>` 的隐藏电源输入引脚VCC，则该引脚在所有图纸上都会全局连接到 `<power_input_pin>`VCC网络。这种隐式连接方式不建议在新设计中使用。

When the power pins of a symbol are visible, they must be connected, as with any other signal. However, symbols are sometimes drawn with hidden power input pins, which are connected implicitly. KiCad automatically connects invisible pins with type Power Input to a global net with the same name as the pin. For example, if a symbol has a hidden power input pin named VCC, this pin will be globally connected to the VCC net on all sheets. This kind of implicit connection is not recommended in new designs.

网络类在原理图设置对话框的“网络类”面板中进行管理 。

Net classes are managed in the Net Classes panel of the Schematic Setup dialog.

顶部窗格列出了设计中存在的网络类。Default 网络类始终存在，您可以使用按钮添加其他网络类 ，也可以使用按钮删除选定的网络类 。

The top pane lists the net classes that exist in the design. The Default net class always exists, and you can add additional net classes with the button or remove the selected net class with the button.

可以使用上下按钮按优先级顺序移动网络类 。 请注意，Default优先级最低的网络类始终是优先级最低的网络类，因此无法移动。

Net classes can be moved up and down in priority order with the and buttons. Note that the Default net class will always be the lowest priority net class and can therefore not be moved.

每个网络类都可以拥有独特的图形属性，这些属性决定了该网络类的导线在原理图中的显示方式。导线和总线的粗细、颜色以及线条样式（实线、虚线、点线等）均可调整。将颜色设置为透明将使用该网络类主题的默认导线/总线颜色，该颜色可在“首选项”中进行配置。默认情况下，为某个网络类配置的任何颜色都将用于绘制该网络类中的导线。如果在“原理图编辑器”首选项的“显示选项”部分启用了“突出显示网络类颜色”设置，则此颜色将用于在该网络类中的导线周围绘制高亮显示，而导线本身将始终使用配色方案的导线颜色绘制。

Each net class can have unique graphic properties that determine how wires of that net class are displayed in the schematic. Wire and bus thicknesses, color, and line style (solid, dashed, dotted, etc.) can all be adjusted. Setting the color to transparent will use the theme’s default wire/bus color for the net class, which is configurable in Preferences. By default any color that is configured for a net class controls the color is used to draw wires in that net class. If the Highlight netclass colors setting is enabled in the Display Options section of the Schematic Editor preferences, this color will instead be used to draw a highlight around wires in that netclass, and the wires themselves will always be drawn with the color scheme’s wire color.

您还可以为每个网络类别设置电路板设计规则，但默认情况下 DRC 字段是隐藏的。右键单击标题行可显示或隐藏其他列。有关设置网络类别设计规则的更多信息，请参阅 PCB 编辑器文档。

You can also set board design rules for each net class, although the DRC fields are hidden by default. Right click the header row to show or hide additional columns. For more information about setting net class design rules, see the PCB editor documentation.

用户自定义网络类的所有网络类参数均为可选。但是，网络类的所有属性都Default必须设置。当一个网络被分配了多个网络类时，图形属性或电路板设计规则的相应值将取自优先级最高且已设置相关值的网络类。如果仅分配了一个网络类，且该网络类包含缺失的属性，则所有缺失值都将取自该Default网络类。

All net class parameters for user-defined net classes are optional. However, all properties belonging to the Default net class must be set. When a net has more than one net class assigned, the appropriate value for graphic properties or board design rules is taken from the highest priority assigned net class with the relevant value set. If only one net class is assigned which contains missing properties, any missing values will be taken from the Default net class.

底部窗格列出了基于模式的网络类别分配。每一行包含一个网络名称模式和一个网络类别；名称与该模式匹配的网络将被分配到指定的网络类别。如果一个网络匹配多个模式，则该网络将被分配到所有匹配的网络类别。您可以单击相应的列标题，按模式或网络类别名称对网络类别分配模式列表进行排序。

The bottom pane lists pattern-based net class assignments. Each row has a net name pattern and a net class; nets with names that match the pattern are assigned to the specified net class. If a net matches multiple patterns, the net is assigned to all of the matching net classes. You can sort the list of net class assignment patterns by pattern or by net class name by clicking on the corresponding column header.

基于模式的网络类别分配是动态的：当添加一个与现有模式匹配的新网络时，它将自动分配到关联的网络类别。网络模式可以使用通配符（`\n`*匹配任意数量的任意字符，包括零个字符；`\n`?匹配任意字符）和 正则表达式。与所选模式匹配的网络将显示在模式列表的右侧。

Pattern-based net class assignments are dynamic: when a new net is added that matches an existing pattern, it will be assigned to the associated net class automatically. Net patterns can use both wildcards (* to match any number of any characters, including none, and ? to match any character) and regular expressions. The nets that match the selected pattern are displayed to the right of the pattern list.

例如，该net*模式匹配名为net、、、以及任何其他以开头的网络名称。因为在正则表达式中，的含义略有不同（匹配零个或多个前面的字符），所以该net1模式也会匹配名为的网络。networknet**net*ne

For example, the net* pattern matches nets named net, net1, network, and any other net name beginning with net. Because * has a slightly different meaning in a regular expression (* matches zero or more of the preceding character), the net* pattern would also match a net named ne.

使用该按钮添加网络类分配模式，或使用该 按钮删除模式。

Use the button to add a net class assignment pattern or the button to remove a pattern.

除了在“原理图设置”对话框中添加网络类别模式外，您还可以直接从原理图画布创建网络类别模式。右键单击一个网络，然后选择“分配网络类别…”以打开“添加网络类别分配” 对话框。网络类别模式会预先填充所选网络的名称，但您可以根据需要更改模式。对话框中会显示所有与该模式匹配的网络。此方法仅适用于已分配名称的网络。

Instead of adding net class patterns in the Schematic Setup dialog, you can directly create net class patterns from the schematic canvas. Right click a net and select Assign Netclass…​ to bring up the Add Netclass Assignment dialog. The net class pattern is pre-filled with the name of the selected net, but the pattern can be changed if desired. All nets matching the pattern are displayed in the dialog. This method can only be used on nets with an assigned name.

作为基于模式的网络类别分配的替代方法，可以使用指令标签、 网络标签或规则区域，以图形方式将网络类别分配给原理图中的网络。

As an alternative to pattern-based net class assignment, net classes can be graphically assigned to nets in the schematic using either directive labels, net labels, or rule areas.

下图中，使用指令标签将信号分配给50R 网络类。

In the image below, a directive label is used to assign signals to the 50R net class.

指令标签通过右侧工具栏中的按钮添加 。它们的作用类似于普通标签，但不能用于命名网络。附加的网络会根据指令Net Class字段的值被分配一个网络类。该字段会显示一个下拉列表，其中包含在原理图设置或 电路板设置Net Class中指定的所有网络类 。

Directive labels are added with the button in the right toolbar. They behave like labels, except that they cannot be used to name a net. The attached net is assigned a net class according to the value of the directive’s Net Class field. The Net Class field presents a dropdown list of all the net classes that have been specified in Schematic Setup or Board Setup.

您还可以输入原理图/电路板设置优先级列表中未明确列出的网络类。此类隐式网络类无法分配任何设计设置，例如网络类颜色或走线宽度，但仍可用于 DRC 规则查询。

You can also type in a net class that isn’t explicitly listed in the Schematic/Board Setup priority list. Such implicit net classes can’t be assigned any design settings, like net class color or track width, but they can still be used in DRC rule queries.

如果Net Class向指令标签添加多个字段，或者Net Class向网络应用多个带有字段的指令标签，则所有指定的网络类都会分配给该网络。

If multiple Net Class fields are added to a directive label, or multiple directive labels with Net Class fields are applied to a net, all of the specified net classes are assigned to the net.

如果将指令附加到总线上，则总线上的所有成员都将被分配到指定的网络类。

If a directive is attached to a bus, all members of the bus are assigned to the specified net class.

除了关联的网络类之外，您还可以在指令的属性中编辑指令的形状 （点、圆、菱形或矩形）、方向、引脚长度和 颜色。

In addition to the associated net class, you can edit the directive’s shape (dot, circle, diamond, or rectangle), orientation, pin length, and color in the directive’s properties.

规则区域工具（）可用于绘制一个形状，并将网络类指令附加到该形状上。任何穿过或位于规则区域内的导线、总线、标签或符号引脚都将被赋予附加到规则区域边界的网络类指令的网络类。下图显示了一个示例；所有穿过规则区域的导线都将被赋予该RAM_ADDR网络类。

The Rule Area tool () can be used to draw a shape to which net class directives can be attached. Any wire, bus, label, or symbol pin which crosses or is inside the rule area will be assigned the net class of a net class directive attached to the rule area border. An example is shown in the image below; all wires passing through the rule area will be assigned the RAM_ADDR net class.

您可以使用“视图” → “显示指令标签”选项在原理图中显示或隐藏指令标签。

You can show or hide directive labels in the schematic using the View → Show Directive Labels option.

示意图中可以添加两种类型的文本，分别称为文本（）和文本框（）。两者都可以通过右侧工具栏中的相应按钮添加。文本框与普通文本类似，区别在于它们可以添加可选边框，并且边框内的文本会自动重排。

Two kinds of text can be added to schematics, which are referred to as text () and text boxes (). Both are added using their respective buttons in the right toolbar. Text boxes are similar to regular text except that they have an optional border and they automatically reflow text within that border.

两种文本项都支持多行文本和基本格式设置功能，但文本框会自动换行以适应边框，并提供额外的格式选项。所有文本均可调整字体、颜色、大小、粗体和斜体、左右对齐以及垂直和水平方向。文本框还支持水平居中、垂直对齐选项以及彩色边框和填充。您还可以调整文本框中文本两侧的内边距（内边距可通过“ 属性管理器”设置，但不能通过“文本框属性”对话框设置）。

Both kinds of text item support multiline text and basic formatting features, but text boxes wrap text to fit in the outline and have additional formatting options. All text has adjustable fonts, color, size, bold and italic emphasis, left and right alignment, and vertical and horizontal orientation. Text boxes additionally support horizontal centering, vertical alignment options, and colored borders and fill. You can also adjust the padding on each side of text in a text box (padding can be set using the Properties Manager, but not using the Text Box Properties dialog).

您可以使用表格以表格形式组织文本。表格的边框、单元格大小、颜色和标题均可自定义。

You can use a table to organize text in a tabular format. Tables have customizable borders, cell sizes, colors, and headers.

要放置表格，请使用右侧工具栏中的按钮。单击画布放置表格的左上角，然后再次单击放置表格的右下角，即可完成表格的绘制。默认情况下，表格越大，添加的行和列就越多，但表格创建完成后，也可以添加或删除行和列。

To place a table, use the button in the right toolbar. Click in the canvas to place the top left corner of the table, then click again to place the bottom right corner of the table and finish drawing the table. The bigger you draw the table, the more rows and columns will be added by default, but rows and columns can be added or deleted after the table is created.

可以使用右侧工具栏中的相应按钮添加图形矩形（）、圆形（）、弧线（）和直线（ ）。

Graphic rectangles (), circles (), arcs (), and lines () can all be added using their respective buttons in the right toolbar.

可以在每个形状的属性对话框中配置线条粗细、颜色和样式（实线、虚线或点线）E。矩形、圆形和弧形还可以设置填充颜色并移除轮廓。

Line width, color, and style (solid, dashed, or dotted) can be configured in the properties dialog for each shape (E). Rectangles, circles, and arcs can also have a fill color set and have their outlines removed.

将图形的线宽设置为 0 将使用原理图的默认线宽，该线宽可在“原理图设置”中进行配置。虚线间距也可在此处配置。移除线条或填充颜色将使用颜色主题的图形颜色，该颜色可在 “首选项”中进行配置。

Setting a shape’s line width to 0 uses the schematic default line width, which is configurable in Schematic Setup. Spacing for line dashes is also configurable there. Removing a line or fill color uses the color theme’s graphics color, which is configurable in Preferences.

与导线类似，图形线条遵循线条绘制模式设置（90 度、45 度或自由角度），您可以使用左侧工具栏上的切换按钮（分别为 、 和 ）进行设置。 + 可 Shift在Space模式之间循环切换。

Like wires, graphic lines obey the line drawing mode setting (90 degree, 45 degree, or free angle), which you can set using the toggle buttons on the left toolbar (, , and , respectively). Shift+Space cycles through the modes.

与 PCB 走线一样， /热键可以切换线路姿态。

As with PCB tracks, the / hotkey switches line posture.

KiCad支持在原理图中插入图像。这些图像仅供设计过程中参考，不具有任何电气功能。

KiCad supports inserting images into the schematic. These are purely for reference during the design process and play no electrical role.

要添加参考图像，请使用右侧工具栏上的按钮并选择所需的参考图像文件。单击画布即可放置图像。

To add a reference image, use the button on the right toolbar and select the desired reference image file. Click in the canvas to place the image.

将图像添加到画布后，您可以使用移动工具（M）或在画布中拖动来重新定位图像。您可以通过拖动图像角点的编辑手柄来缩放图像。图像会围绕其参考点进行缩放；换句话说，参考点是图像中始终保持在画布上同一位置的点，无论图像如何缩放。参考点显示为第五个编辑手柄。它最初位于图像中心，但您可以通过在画布中拖动来重新定位参考点。

Once the image has been added to the canvas, you can reposition it using the move tool (M) or by dragging it in the canvas. You can scale it by dragging the editing handles at the corners of the image. The image is scaled around its reference point; in other words, the reference point is the point in the image that always stays in the same position in the canvas, no matter how the image is scaled. The reference point is shown as a fifth editing handle. Initially it is at the center of the image, but you can reposition the reference point by dragging it in the canvas.

您还可以在图像属性对话框 ( ) 中重新定位或缩放图像。您可以在“常规”E选项卡中设置图像的精确X和Y坐标，并在“图像”选项卡中设置精确的缩放比例。您也可以 根据需要将其转换为灰度图像。此对话框中的位置和缩放是相对于图像中心而非其交互式参考点而言的。

You can also reposition or scale the image in its properties dialog (E). You can set the image’s exact Position X and Y in the General tab, and set an exact Scale factor in the Image tab. You can also Convert to Greyscale if you wish. Position and scale in this dialog are relative to the center of the image, not its interactive reference point.

可以使用“编辑文本和图形属性”对话框（编辑→编辑文本和图形属性… ）批量编辑文本和图形（包括符号字段）的属性。该工具还可以修改导线和总线的视觉属性。

Properties of text and graphics, including symbol fields, can be edited in bulk using the Edit Text and Graphic Properties dialog (Edit → Edit Text and Graphic Properties…​). The tool can also modify visual properties of wires and buses.

图纸标题栏可以使用“页面设置”工具进行编辑（）。您也可以双击图纸上任意位置来打开此工具。

The drawing sheet’s title block is edited with the Page Settings tool (). You can also open this tool by double clicking anywhere on any part of the drawing sheet.

标题栏中的每个字段以及纸张尺寸和方向均可编辑。如果选中某个字段的“导出到其他纸张”选项，则该字段将在所有纸张的标题栏中更新，而不仅仅是当前纸张。

Each field in the title block can be edited, as well as the paper size and orientation. If the Export to other sheets option is checked for a field, that field will be updated in the title block of all sheets, rather than only the current sheet.

您可以通过按“发布日期”旁边的左箭头按钮，将日期设置为今天或其他任何日期。请注意，原理图标题栏中列出的日期不会自动更新，只有在此对话框中更改后才会更新。

You can set the date to today’s or any other date by pressing the left arrow button next to Issue Date. Note that the date listed in the schematic title block is not automatically updated. It is only updated when changed in this dialog.

您还可以选择图纸文件来替换默认图纸。选择图纸时，您可以在文件浏览器中启用“嵌入文件”复选框，将图纸嵌入到原理图中，而不是引用外部文件。这意味着，即使原理图在另一台计算机上打开，而该计算机上的图纸文件不在相同的外部路径下，原理图的显示效果也与原图相同。有关更多信息，请参阅 嵌入文件文档。

A drawing sheet file can also be selected to replace the default drawing sheet. When choosing a drawing sheet, you can enable the Embed File checkbox in the file browser to embed the drawing sheet in the schematic instead of referencing an external file. This means the schematic will appear the same when it is opened on another computer that does not have the drawing sheet file available at the same external file path. For more information, see the embedded files documentation.

图纸编号（图纸 X/Y）会自动更新，但也可以使用“编辑→编辑图纸页码…”手动设置图纸页码。

The sheet number (Sheet X/Y) is automatically updated, but sheet page numbers can also be manually set using Edit → Edit Sheet Page Number…​.

您可以使用右键菜单中的 “引脚助手”工具，快速为选定的引脚添加导线、标签或未连接标记。这有助于您快速从符号或层级图中分离出未连接的引脚。选择“引脚助手” → “导线”，导线工具将一次性从所有选定的引脚绘制导线。如果选择“未连接”，则会在每个选定引脚的末端添加未连接标记。如果选择“网络标签”、 “层级标签”或“全局标签”，则会在每个选定引脚的末端放置相应类型的标签。每个标签的名称将设置为相应的引脚名称。新标签将保持选中状态，因此您可以根据是否希望保持引脚和标签之间的连接，使用“移动M”或“删除”按钮轻松地将它们从符号中移开。G

You can quickly add wires, labels, or no-connection markers to a selection of pins using the Pin Helpers tools in the right-click context menu. This can help you quickly break out unconnected pins from a symbol or hierarchical sheet. By selecting Pin Helpers → Wire, the wire tool will begin drawing a wire from all selected pins at once. If you select No Connect, no-connection markers will be added to the end of each selected pin. And if you choose Net Label, Hierarchical Label, or Global Label, a label of the respective type will be placed at the end of each selected pin. Each label’s name will be set to the corresponding pin name. The new labels will remain selected, so you can easily move them away from the symbol using M or G, depending on whether you wish to maintain a wired connection between the pins and the labels.

可以通过右键单击现有标签和文本对象，然后从“更改为”子菜单中选择目标对象类型，将其更改为其他类型的标签或文本。源对象和目标对象允许的类型包括：本地标签、全局标签、层级标签、指令标签、文本对象和文本框。原始对象的值会在结果对象中保留：当文本对象转换为标签时，标签的值（网络名称）将是原始文本，反之亦然。

Existing labels and text objects can be changed to another type of label or text by right clicking the object(s) and selecting the target object type from the Change To submenu. The allowed types for source and target objects are local labels, global labels, hierarchical labels, directive labels, text objects, and text boxes. The value of the original object is preserved in the resulting object: when a text object is converted to a label, the label’s value (net name) will be the original text, and vice versa.

Alt您可以使用“交换”命令（ +S ；也可在右键菜单中找到）交换两个选定对象的位置。此命令适用于许多原理图元素，包括符号、符号字段、标签、图形元素和文本。第一个对象的位置和旋转角度将变为第二个对象的位置和旋转角度，反之亦然。如果选择了两个以上的对象，则位置会循环：最后一个对象获得第一个对象的位置，第一个对象获得第二个对象的位置，依此类推。

You can swap the position of two selected objects using the Swap command (Alt+S; also available in the right-click context menu). This works on many schematic items, including symbols, symbol fields, labels, graphical items, and text. The first object is assigned the location and rotation of the second object, and vice versa. If there are more than two objects selected, the locations are cycled: the last object gets the position of the first object, the first object gets the location of the second, and so on.

格式设置面板包含符号、文本、标签、图形和线条外观的设置。

The formatting panel contains settings for the appearance of symbols, text, labels, graphics, and wires.

符号单元表示法规定了多单元符号中每个单元在其参考标识符中的表示方式。默认情况下，每个单元都用不同的字母附加到参考标识符后，且不加分隔符，例如U1B符号的第二个单元U1，但此设置可以更改。可以使用数字代替字母，并且可以在符号标识符和单元标识符之间使用各种分隔符（例如.，` \n` -、`\n` _、`\n` 或不使用分隔符）。

Symbol unit notation sets how each unit of a multi-unit symbol is referred to in its reference designator. By default, a different letter for each unit is appended to the reference designator with no separator, for example U1B for the second unit of symbol U1, but this can be changed. Numbers can be used instead of letters, and various separators can be used between the symbol designator and the unit identifier (., -, _, or none).

默认文本大小设置文本、文本框和标签工具使用的默认文本高度。上标偏移比例控制文本与其上方的上标 ( ~{}) 之间的垂直间距，该比例为文本高度的百分比。 标签偏移比例控制本地标签文本与其连接的导线之间的垂直间距，该比例相对于标签文本大小。这也会影响符号引脚与其引脚编号之间的间距。全局标签边距比例 定义全局标签周围边框的大小，该比例相对于全局标签的文本大小。增加边距有助于避免文本与上标 ( ~{}) 或带有下延部分的字母重叠，但这可能会导致紧密排列的全局标签相互重叠。

Default text size sets the default text height used by the text, text box, and label tools. Overbar offset ratio controls the vertical spacing between text and an overbar (~{}) over that text, as a ratio of the text height. Label offset ratio controls the vertical spacing between a local label’s text and the attached wire, relative to the label’s text size. This also affects the spacing between symbol pins and their pin number. Global label margin ratio defines the size of the box around a global label, relative to the global label’s text size. Increasing the margin may be useful to avoid overlapping text with overbars (~{}) or letters with descenders, but this may cause closely packed global labels to overlap with each other.

默认线宽设置符号图形的默认线宽（如果符号未覆盖默认线宽）。引脚符号大小缩放符号引脚图形样式注释，例如倒置引脚上的气泡。

Default line width sets the default line width for symbol graphics, if the symbol does not override the default line width. Pin symbol size scales symbol pin graphic style annotations, such as the bubble on an inverted pin.

连接点大小设置原理图中的默认导线连接点大小。可以通过编辑单个连接点的属性来覆盖默认大小。连接宽度指定用于 符号引脚或导线末端连接网格ERC 检查的网格大小。原理图通常使用 50 mil 的网格进行电气连接，因此此值通常应保持设置为 50 mil。

Junction dot size sets the schematic’s default wire junction dot size. The default size can be overridden by editing an individual junction dot’s properties. Connection width specifies the grid size used for the Symbol pin or wire end off connection grid ERC check. Schematics typically use a 50 mil grid for electrical connections, so this should usually remain set at 50 mils.

工作点叠加设置用于配置 工作点仿真注释在原理图画布上的显示方式。有效数字设置控制电压和电流叠加层上打印的有效数字位数。范围设置控制用于显示电压和电流测量值的单位。

The Operating Point Overlay settings configure how operating point simulation annotations are displayed on the schematic canvas. The significant digits settings control the number of significant digits printed on voltage and current overlays. The range settings control the units used to display voltage and current measurements.

“显示页间引用”选项启用或禁用页间引用的显示 。页间引用是指全局标签旁边的一系列页码，这些页码链接到原理图中其他出现相同全局标签的位置。“显示本页引用”选项控制当前页是否包含在页码列表中。“标准”和 “缩写”选项决定是显示完整的页码列表，还是仅显示首尾页码。“前缀”和“后缀”字段用于在页码列表前后添加可选字符。在下面的页间引用示例中，分别添加了前缀“1”和后缀“ [2 ”。]

Show inter-sheet references enables or disables the display of inter-sheet references, which are a list of page numbers next to a global labels that link to other places in the schematic where the same global label appears. Show own page reference controls whether the current page is included in the list of page numbers. Standard and abbreviated determine whether to display the complete list of page numbers or only the first and last page numbers. The prefix and suffix fields add optional characters before and after the list of page numbers. In the image of an inter-sheet reference below, a prefix and suffix of [ and ], respectively, have been added.

虚线的外观在“格式”部分进行控制。“虚线长度” 控制虚线的长度，“间距长度”控制虚线和点之间的间距。虚线和间距的长度与线宽相关：间距长度为 22表示间距长度为线宽的两倍。

Dashed line appearance is controlled in the Formatting section. Dash length controls the length of dashes, while Gap length controls the spacing between dashes and dots. The dash and gap lengths are relative to the line width: a gap length of 2 means twice the width of the line.

字段名称模板是自动添加到原理图所有符号的空符号字段。当原理图中的每个符号都需要库符号中未定义的字段之外的其他字段时，例如制造商零件编号字段，这些模板非常有用。

Field name templates are empty symbol fields that are automatically added to all symbols in the schematic. These can be useful when every symbol in the schematic needs additional fields beyond the fields that are defined in the library symbols, for example a field for the manufacturer’s part number.

模板字段可以设置为可见或不可见，也可以设置为 URL 字段。

Template fields can be set as visible or invisible, and can also be set as URL fields.

在原理图设置中定义的字段名称模板仅适用于当前项目。也可以在“首选项”中定义字段名称模板 ，这些模板将应用于计算机上编辑的所有项目。

Field name templates that are defined in schematic setup apply only to the current project. Field name templates can also be defined in Preferences, which apply to all projects edited on your computer.

BOM预设是 符号字段表和BOM导出工具的已保存配置。预设分为两种类型：BOM预设用于配置符号字段表中显示的字段、它们的显示顺序以及如何使用它们对符号进行分组。这些字段也会直接用于BOM输出。BOM格式预设用于配置输出BOM文件的格式，包括用于分隔字段的分隔符。两种类型的预设都在符号字段表中创建，但可以在此处列出和删除。

BOM presets are saved configurations for the Symbol Fields Table and BOM export tool. There are two types of presets. BOM presets configure which fields are displayed in the symbol fields table, which order they are displayed in, and how they are used to group symbols. These fields are also directly used in the BOM output. BOM formatting presets configure the output BOM file format, including which separator characters are used to separate fields. Both types of presets are created in the Symbol Fields Table, but can are listed and can be deleted here.

“违规严重性”面板允许您配置应将哪些类型的 ERC 消息报告为错误、警告或忽略。

The Violation Severity panel lets you configure what types of ERC messages should be reported as Errors, Warnings, or ignored.

引脚冲突映射表允许您配置连接规则，根据相互连接的引脚类型定义错误和警告的电气条件。例如，默认情况下，当一个输出引脚连接到另一个输出引脚时会产生错误。

The Pin Conflicts Map allows you to configure connectivity rules to define electrical conditions for errors and warnings based on what types of pins are connected to each other. For example, by default an error is produced when an output pin is connected to another output pin.

这些面板在ERC 部分有更详细的解释。

These panels are explained in more detail in the ERC section.

“网络类别”面板允许您管理项目的网络类别，并使用模式将网络分配给相应的网络类别。在此面板中管理网络类别与在 “电路板设置”对话框中管理网络类别的功能相同。您还可以使用网络类别指令或 网络标签，通过图形化分配的方式在原理图中将网络分配给相应的网络类别。

The Net Classes panel allows you to manage net classes for the project and assign nets to net classes with patterns. Managing net classes in this panel is equivalent to managing them in the Board Setup dialog. Nets can also be assigned to net classes in the schematic using graphical assignments with net class directives or net labels.

基于模式的网络类分配在网络类部分有更详细的解释 。

Pattern-based net class assigment is explained in more detail in the net classes section.

“总线别名定义”面板允许您创建总线别名，总线别名是总线中信号组的名称。有关总线别名的更多信息，请参阅总线别名文档。

The Bus Alias Definitions panel allows you to create bus aliases, which are names for groups of signals in a bus. For more information about bus aliases, see the bus alias documentation.

可以在“文本变量”部分创建文本变量。KiCad 会将变量名替换为分配给该变量的文本字符串。无论变量名出现在变量替换语法中的哪个位置，都会发生这种替换${VARIABLENAME}。

Text variables can be created in the Text Variables section. KiCad will substitute the variable name with the text string assigned to the variable. This substitution happens anywhere the variable name is used inside the variable replacement syntax of ${VARIABLENAME}.

例如，您可以创建一个名为 `<variable>` 的变量VERSION，并将其文本替换设置为 `<variable> 1.0`。现在，在原理图中的任何文本对象中，您都可以输入 ` <variable> ${VERSION}`，KiCad 会将其显示为 `<variable>` 1.0。如果您将 `<variable>` 的值更改为 `<variable>` 2.0，则所有包含 `<variable>` 的文本对象${VERSION}都会自动更新。您还可以混合使用普通文本和变量。例如，您可以创建一个文本对象，其中包含文本 `<variable>`，Version: ${VERSION}该文本将显示为 `<variable>` Version: 1.0。

For example, you could create a variable named VERSION and set the text substitution to 1.0. Now, in any text object in the schematic, you can enter ${VERSION} and KiCad will display this as 1.0. If you change the value to 2.0, every text object that includes ${VERSION} will be updated automatically. You can also mix regular text and variables. For example, you can create a text object with the text Version: ${VERSION} which will be displayed as Version: 1.0.

也可以在电路板设置中创建文本变量 。文本变量是项目范围内的；在原理图编辑器中创建的变量也可以在电路板编辑器中使用，反之亦然。

Text variables can also be created in Board Setup. Text variables are project-wide; variables created in the schematic editor are also available in the board editor, and vice versa.

此外，还有一些内置的系统文本变量。

There are also a number of built-in system text variables.

外部文件可以嵌入到原理图中。嵌入文件会将文件的副本存储在原理图文件中。这样，设计就可以引用嵌入的文件副本，而无需依赖外部文件，从而使项目更具可移植性。字体、数据手册、绘图纸、SPICE 模型和封装 3D 模型都可以嵌入到 KiCad 中使用。其他任意文件也可以嵌入到项目中，以便稍后导出，但 KiCad 的任何功能都不会使用这些文件。嵌入到原理图中的文件必然会增加原理图文件的大小，尽管文件在嵌入之前会进行压缩以尽量减少所需的空间。

External files can be embedded within a schematic. Embedding a file stores a copy of the file inside the schematic file. The design can then refer to the embedded copy of the file instead of the external file, which makes the project more portable as it doesn’t rely on an external file. Fonts, datasheets, drawing sheets, SPICE models, and footprint 3D models can be embedded and used within KiCad. Other arbitrary files can also be embedded to store them in the project for later export, but they are not used by any KiCad functionality. Files embedded in a schematic necessarily increase the schematic’s file size, although files are compressed before being embedded to minimize the space required.

嵌入文件在原理图设置的“嵌入文件”部分进行管理。原理图中嵌入的所有文件都会显示在此处。要将文件嵌入原理图，请单击按钮 并选择该文件。文件随后会被嵌入原理图，并与其嵌入引用一起列在嵌入文件列表中。嵌入引用是嵌入文件的唯一标识符，以“.”开头kicad-embed://。您可以在原理图编辑器中的其他位置使用此嵌入引用，就像引用外部文件路径一样。您可以通过右键单击并选择“复制嵌入引用”来复制嵌入引用。要删除嵌入文件，请单击按钮。指向已删除文件的所有剩余链接都将失效。

Embedded files are managed in the Embedded Files section of Schematic Setup. All files embedded in a schematic are shown here. To embed a file inside a schematic, click the button and select the file. The file is then embedded inside the schematic and is listed in the embedded files list along with its embedded reference. The embedded reference is a unique identifier for the embedded file that begins with kicad-embed://. You can use the embedded reference elsewhere in the Schematic Editor to refer to the embedded file as if it were an external file path. You can copy the embedded reference by right clicking and selecting Copy Embedded Reference. To remove an embedded file, click the button. Any remaining links to the removed file will become invalid.

要在原理图中使用的任何字体中嵌入字体，请选中“嵌入字体”复选框。原理图中使用的所有字体都将被嵌入，因此无论字体文件是否已安装，都可以在任何计算机上编辑使用该字体的文本。

To embed any fonts used in a schematic, check the Embed fonts checkbox. All fonts used in the schematic will be embedded, so text using that font can be edited on any computer regardless of whether the font file is installed.

您还可以将文件嵌入库符号中。此类文件可在符号内部访问，但无法在更大的原理图或其他符号中使用。将符号添加到原理图时，嵌入在符号中的文件会被去重：如果一个文件嵌入在一个符号中，并且该符号的多个实例被添加到原理图中，则只会嵌入该文件的一个副本，所有符号实例都将引用同一个嵌入的文件。

You can also embed files in a library symbol. Such files will be available within the symbol, but not within the larger schematic or in other symbols. Files embedded in a symbol are deduplicated when the symbol is added to a schematic: if a file is embedded in a symbol, and multiple instances of that symbol are added to the schematic, only one copy of the file will be embedded, and all of the symbol instances will refer to the same embedded file.

例如，要将数据手册嵌入到项目中并在多个符号中使用它，您可以使用原理图设置对话框嵌入数据手册，复制内部引用，然后将内部引用粘贴到每个使用该数据手册的符号的数据手册字段中。这样，每个符号就都拥有了对嵌入数据手册的通用引用。或者，您可以将数据手册嵌入到库符号中。在这种情况下，当符号添加到原理图时，每个符号都已嵌入了数据手册。不过，实现相同目的的更便捷方法是打开符号的属性对话框，浏览并找到数据手册文件，然后在文件浏览器中启用“嵌入文件” 选项。同样，这可以应用于原理图中的符号，也可以应用于源符号库中的符号。

As an example, to embed a datasheet in a project and use it within several symbols, you could embed the datasheet using the schematic setup dialog, copy the internal reference, and paste the internal reference into the datasheet field of each symbol that uses that datasheet. Each symbol would then have a portable reference to the embedded datasheet. Alternatively, you could embed the datasheet within the library symbol. In this case, each symbol will already have the datasheet embedded when the symbol is added to a schematic. A more convenient way to achieve the same thing, however, is to open the symbol’s properties dialog, browse for a datasheet file, and enable the Embed File option in the file browser. Again, this could be done for a symbol in the schematic or for a symbol in the source symbol library.

文件也可以嵌入到电路板中。

Files can also be embedded in boards.

您可以从现有原理图中导入部分或全部原理图设置。这样，您可以选择一个原理图用作模板，并选择要导入的设置。

You can import some or all of the schematic setup from an existing schematic. This allows you to choose a schematic to use as a template and select which settings to import.

要导入设置，请单击“原理图设置”对话框底部的“从其他项目导入设置…”.kicad_sch按钮，然后选择 要从中导入的文件。选择要导入的设置，当前设置将被所选原理图中的值覆盖。

To import settings, click the Import Settings from Another Project…​ button at the bottom of the Schematic Setup dialog and then choose the .kicad_sch file you want to import from. Select which settings you want to import and the current settings will be overwritten with the values from the chosen schematic.

可导入的设置包括：

The settings that are available to import are:

<projectname>-cache.lib现代版本的 KiCad 可以打开在 KiCad 6.0 之前的版本中创建的原理图，但必须存在缓存库文件（ ）才能正确加载原理图。

Modern versions of KiCad can open schematics created in versions prior to KiCad 6.0, but the cache library file (<projectname>-cache.lib) must be present to load the schematic correctly.

自 6.0 版本起，KiCad 会将项目中使用的所有符号存储在原理图中。这意味着，即使项目中使用的库未安装或已更改，您也可以在任何计算机上打开使用 KiCad 6.0 或更高版本创建的原理图。现代 KiCad 原理图文件使用 .kbd.kicad_sch扩展名。

Since version 6.0, KiCad stores all symbols used in a project in the schematic. This means that you can open a schematic made in KiCad 6.0 or later on any computer, even if the libraries used in the project are not installed or have changed. Modern KiCad schematic files use the .kicad_sch extension.

在 6.0 版本之前，KiCad 并不直接在原理图中存储符号。相反，KiCad 存储的是符号及其库的引用。它还会将项目使用的每个符号的副本存储在一个单独的缓存库文件中（<projectname>-cache.lib）。只要项目中包含了缓存库，就可以在不包含系统库文件的情况下分发项目，因为如果原理图中引用的库文件缺失，KiCad 可以从缓存库中加载任何所需的符号作为备用方案。旧版 KiCad 原理图文件使用 .kbd.sch扩展名。

Prior to version 6.0, KiCad did not store symbols in the schematic. Instead, KiCad stored references to the symbols and their libraries. It also stored a copy of every symbol used by the project in a separate cache library file (<projectname>-cache.lib). As long as the cache library was included with the project, the project could be distributed without the system library files, because KiCad could load any needed symbols from the cache library as a fallback if the libraries referenced in the schematic were missing. Legacy KiCad schematic files use the .sch extension.

打开旧版原理图时，KiCad 会在缓存库中查找原理图中使用的所有符号。保存旧版原理图时，KiCad 会将其另存为现代原理图格式的新文件.kicad_sch，并将必要的符号嵌入到原理图本身中。原始的旧版原理图和缓存库将保持不变，但原理图保存为现代格式后，它们就不再需要了。

When you open a legacy schematic, KiCad will look in the cache library to find all of the symbols used in the schematic in the cache library. When you save the legacy schematic, KiCad will save it as a new file in the modern schematic format (.kicad_sch), with the necessary symbols embedded in the schematic itself. The original legacy schematic and the cache library will remain, unmodified, but they are no longer necessary once the schematic has been saved in the modern format.

打开旧版原理图时，KiCad 可能会显示“项目修复助手”对话框。这意味着缓存库中的一个或多个符号与外部库中的对应符号不匹配。如果需要，此对话框可帮助您将缓存库中的符号“修复”到原理图中。您也可以随时使用“工具” → “修复符号…”打开此修复对话框。使用此修复工具必须存在缓存库文件。

When you open a legacy schematic, KiCad may display the Project Rescue Helper dialog. This means that one or more symbols in the cache library do not match the corresponding symbol in the external library. The dialog helps you "rescue" symbols from the cache library into your schematic, if desired. You can also open the rescue dialog at any time using Tools → Rescue Symbols…​. The cache library file must be present in order to use the rescue tool.

救援对话框会列出缓存库和外部符号库中所有不匹配的符号。造成这种差异的原因可能是：

The rescue dialog lists all symbols that don’t match between the cache library and the external symbol library. The discrepancy can be because:

对于列表中的每个符号，选中该符号后，对话框会显示该符号每个实例的引用指示符和值，并显示该符号的预览。如果系统符号库中存在对应的符号，对话框会同时显示这两个符号副本以进行比较。如果该符号仅存在于缓存库中，对话框则仅显示缓存的符号。

For each symbol in the list, selecting the symbol displays the reference designator and value for each instance of the symbol, and shows a visual preview of the symbol. If a corresponding symbol exists in the system symbol library, the dialog shows both copies of the symbol for comparison. If the symbol only exists in the cache library, the dialog only shows the cached symbol.

在这个例子中，项目最初使用的是阴极朝左的二极管，但库中现在包含的二极管阴极朝右。这一更改会破坏设计，因此务必按照原始设计者的意图使用缓存的符号。

In this example, the project originally used a diode with the cathode facing left, but the library now contains one with the cathode facing right. This change would break the design, so it would be important to use the cached symbol as the original designer intended.

在此处按下“恢复符号”按钮，会将缓存库中选定的符号保存到一个特殊rescue库中（<projectname>-rescue.kicad_sym）。原理图中的相应符号将更新为使用新恢复的符号。任何未选中的符号都不会被恢复，但稍后可以在原理图中更新它们的符号链接。

Pressing Rescue Symbols here will cause the selected symbols from the cache library to be saved into a special rescue library (<projectname>-rescue.kicad_sym). The corresponding symbols in the schematic will be updated to use the newly rescued symbols. Any unselected symbols will not be rescued, but their symbol linkage can be updated in the schematic later.

或者，按下“跳过符号恢复”按钮将退出对话框而不恢复任何符号。KiCad 将使用外部库中找到的符号版本。您可以再次运行恢复功能（使用“工具” → “恢复符号…”），或者在符号属性中手动编辑符号链接。

Alternatively, pressing Skip Symbol Rescue will exit the dialog without rescuing any symbols. KiCad will use the versions of the symbols found in the external libraries. You can run the rescue function again with Tools → Rescue Symbols…​, or manually edit symbol linkage in the symbol’s properties.

如果您不想再看到此对话框，可以按“不再显示” 。这与按“跳过符号救援”按钮的效果相同，该按钮将对当前原理图和所有后续原理图都有效。

If you would prefer not to see this dialog, you can press Never Show Again. This has the same effect as pressing Skip Symbol Rescue for the current schematic and all future schematics.

如果旧版原理图中的某个符号在缓存库或外部库中都找不到，KiCad 将无法恢复该符号。此时，原理图中会插入一个占位符符号来代替它，如下所示。

If a symbol in a legacy schematic cannot be found in either the cache library or the external library, KiCad cannot rescue that symbol. A placeholder symbol is inserted into the schematic in its place, as shown below.

您可以使用“更改符号”或 “编辑符号库链接”对话框尝试重新映射这些孤立的符号，但这两种方法都可能需要手动修正原理图。有关这些工具的详细说明，请参阅“更新和交换符号”部分。

You can attempt to remap these orphaned symbols using the Change Symbols or Edit Symbol Library Links dialogs, but either option may require manual corrections to the schematic. These tools are explained in more detail in the Updating and exchanging symbols section.

现代版本的 KiCad 可以打开在 KiCad 5.0 之前的版本中创建的原理图，但您需要进行符号重映射过程才能在不丢失符号信息的情况下打开原理图。

Modern versions of KiCad can open schematics created in versions prior to KiCad 5.0, but you will need to go through a symbol remapping process to open the schematic without losing symbol information.

自 5.0 版本起，KiCad 原理图使用符号名称和库名称来指代特定符号。即使多个库中都包含同名符号，设计者想要使用的符号也能被明确指定。

Since version 5.0, KiCad schematics refer to specific symbols using both the symbol and library name. Even if multiple libraries each contain a symbol with the same name, the designer’s intended symbol is unambiguously specified.

在 5.0 版本之前，KiCad 原理图仅存储符号名称，而不存储库名称。原理图中的符号是通过在项目的库列表中搜索匹配的符号，间接映射到原始库的。当您打开 5.0 版本之前的原理图时，KiCad 会尝试自动“重新映射”符号，将每个裸符号名称替换为完整的符号库和符号名称对。原始原理图将备份到一个rescue-backup文件夹中。

Prior to version 5.0, KiCad schematics stored only the symbol name, not the library name. Symbols in the schematic were indirectly mapped back to the original library by searching through the project’s library list for a matching symbol. When you open a pre-5.0 schematic, KiCad will attempt to automatically "remap" the symbols so that each bare symbol name is replaced with a fully-specified symbol library and symbol name pair. The original schematics will be backed up in a rescue-backup folder.

您可以跳过自动重映射，但需要使用“更改符号”对话框自行重映射符号。您也可以使用“工具” → “重映射旧版库符号…”重新运行“重映射符号”工具。

You can skip the automatic remapping, but you will need to remap the symbols yourself using the Change Symbols dialog. You can also re-run the Remap Symbols tool using Tools → Remap Legacy Library Symbols…​.

图纸之间的电气连接通过标签实现。KiCad 中有几种标签，每种标签的连接范围都不同。

Electrical connections between sheets are made with labels. There are several kinds of labels in KiCad, each with a different connection scope.

在子图纸中放置层级标签后，即可在父图纸中的子图纸符号中添加匹配的层级图纸引脚。然后，您可以使用导线、标签和总线将层级引脚连接到子图纸符号。子图纸符号中的层级图纸引脚与子图纸本身中匹配的层级标签相连。

After placing hierarchical labels within the subsheet, matching hierarchical sheet pins can be added to the subsheet symbol in the parent sheet. You can then make connections to the hierarchical pins with wires, labels, and buses. Hierarchical sheet pins in a subsheet symbol are connected to the matching hierarchical labels in the subsheet itself.

对于子图纸中的每个层级标签，单击 右侧工具栏中的按钮，然后单击图纸符号，即可将相应的层级图钉添加到图纸符号上。第一个未匹配的层级标签对应的图钉将附加到光标处，您可以将其放置在图纸符号边界上的任意位置。再次单击该工具将继续添加图钉，直到子图纸中的所有层级标签都在图纸符号上拥有匹配的图钉为止。您也可以通过在图纸符号的右键菜单中选择“放置图钉”来导入图钉。

For every hierarchical label in the subsheet, add the corresponding hierarchical pin onto the sheet symbol by clicking the button in the right toolbar, then clicking on the sheet symbol. A sheet pin for the first unmatched hierarchical label will be attached to the cursor, where it can be placed anywhere along the border of the sheet symbol. Clicking again with the tool will continue to add additional sheet pins until all of the hierarchical labels in the subsheet have a matching sheet pin on the sheet symbol. Sheet pins can also be imported by selecting Place Sheet Pin in a sheet symbol’s right-click context menu.

您可以在“图钉属性”对话框中编辑图钉的属性。双击图钉、选择图钉并使用E快捷键、或右键单击图钉并选择 “属性…”即可打开此对话框。

You can edit the properties of a sheet pin in the Sheet Pin Properties dialog. Open this dialog by double-clicking a sheet pin, selecting a sheet pin and using the E hotkey, or right-clicking a sheet pin and selecting Properties…​.

可以在文本框中编辑图纸图钉名称，也可以从子图纸的层级标签下拉列表中选择。图纸图钉名称必须与子图纸中对应的层级标签名称一致，因此如果更改图钉名称，则必须同时更改标签名称。

The sheet pin’s name can be edited in the textbox or by selecting from the dropdown list of hierarchical labels in the subsheet. A sheet pin’s name has to match the corresponding hierarchical label in the subsheet, so if you change a pin name you must change the label name as well.

形状设置会改变引脚的形状，但不会影响其电气特性。它可以设置为输入、输出、双向、三态或被动模式。引脚的字体、字号、颜色和强调方式（粗体或斜体）也可以更改。

Shape changes the shape of the sheet pin, and has no electrical effect. It can be set to Input, Output, Bidirectional, Tri-state, or Passive. The pin’s font, text size, color, and emphasis (bold or italic) can also be changed.

管理层级标签和图纸图钉之间连接的另一种方法是使用“同步图纸图钉”工具。可以通过 右侧工具栏中的按钮启动此工具，也可以在图纸符号的右键菜单中选择“同步图纸图钉”来启动。

Another way to manage the connections between hierarchical labels and sheet pins is to use the Sync Sheet Pins tool. Launch this tool using the button in the right toolbar or with Sync Sheet Pins in a sheet symbol’s right click context menu.

此对话框显示每个层级图纸的层级标签和层级图纸图钉。如果该工具是从图纸符号的上下文菜单启动的，则只会显示一个选项卡，其中包含该特定图纸的标签和图钉。如果该工具是全局启动的，例如通过按钮 或“放置” → “同步图钉”，则会为每个层级图纸显示一个选项卡。

This dialog shows the hierarchical labels and hierarchical sheet pins for each hierarchical sheet. If the tool was launched from the context menu of a sheet symbol, only one tab will be available, with the labels and sheet pins for that specific sheet. If the tool was started globally, i.e. with the button or with Place → Sync Sheet Pins, a tab will be shown for each hierarchical sheet.

每个选项卡中的图标指示图纸符号上的层级引脚是否与图纸内的层级标签正确匹配。如果选项卡中有图标，则表示图纸中存在一个没有匹配引脚的层级标签，或者一个没有对应层级标签的引脚，或者两者兼有。如果选项卡中有 图标，则表示层级标签和层级引脚已正确匹配。如果引脚和标签具有相同的名称和相同的图形形状（输入、输出、双向、三态或被动），则认为它们匹配。

The icon in each tab indicates whether the hierarchical sheet pins on the sheet symbol are correctly matched with the hierarchical labels inside the sheet. If the tab has a icon, then there is a hierarchical label in the sheet without a matching sheet pin, or a sheet pin without a corresponding hierarchical label, or both. If the tab has a icon, then the hierarchical labels and hierarchical sheet pins are matched up correctly. Sheet pins and labels are considered matching if they have the same name and the same graphic shape (input, output, bidirectional, tri-state, or passive).

左侧一列列出了当前图纸中没有对应层级标签的图纸图钉。中间一列列出了当前图纸中没有对应层级图钉的层级标签。右侧一列列出了匹配的图纸图钉和层级标签。每个图钉或标签的名称及其图形形状均会显示。

The column on the left lists sheet pins for the current sheet that do not have a corresponding hierarchical label in the sheet. The middle column lists hierarchical labels in the current sheet that do not have a corresponding hierarchical sheet pin on the sheet symbol. The right column lists pairs of matching sheet pins and hierarchical labels. The name of each pin or label is shown along with its graphic shape.

单击“添加层级标签”按钮，系统将为所选图纸图钉创建新的层级标签，供您按顺序放置在图纸中。选定的图纸图钉将从左侧列中移除，并添加到右侧列，以便与标签匹配。单击“删除图纸图钉”按钮将从图纸符号中删除选定的图纸图钉。

If you click the Add Hierarchical Labels button, new hierarchical labels corresponding to the selected sheet pins will be created for you to place sequentially in the sheet. The selected sheet pins are then removed from the left column and added to to the right column for matching sheet pins and labels. Clicking Delete Sheet Pins will delete the selected sheet pins from the sheet symbol.

单击“添加图纸图钉”按钮，系统将创建与所选层级标签对应的新图纸图钉，供您放置在图纸符号上。然后，层级标签将从中间列移除并添加到右侧列，以便与对应的图纸图钉和标签进行匹配。单击“删除层级标签”将从图纸中删除所选的层级标签。

If you click the Add Sheet Pins button, new sheet pins corresponding to the selected hierarchical labels will be created for you to place on the sheet symbol. The hierarchical labels are then removed from the middle column and added to the right column for matching sheet pins and labels. Clicking Delete Hierarchical Labels will delete the selected hierarchical labels from inside the sheet.

点击该按钮会将选定的图纸图钉与层级标签匹配，方法是将图纸图钉重命名为与层级标签名称一致。点击该 按钮则会执行相反的操作，将选定的图纸图钉与层级标签匹配，方法是将层级标签重命名为与图纸图钉名称一致。

Clicking the button will match the selected sheet pin and hierarchical label by renaming the sheet pin to match the hierarchical label’s name. Clicking the button will do the opposite, matching the selected sheet pin and hierarchical label by renaming the label to match the sheet pin.

点击该按钮将取消已匹配的元素对，并将图纸图钉和层级标签都移回各自的未匹配列。之后，可以根据需要编辑或重新匹配未匹配的图纸图钉和层级标签。

Clicking the button will unmatch a matched pair, moving both the sheet pin and the hierarchical label back to their respective unmatched columns. The unmatched sheet pin and hierarchical label can then be edited or rematched as desired.

在“同步工作表图钉”对话框中所做的任何更改都会立即生效，甚至在对话框关闭之前就会生效。要取消在“同步工作表图钉”对话框中所做的更改，请使用“撤消”功能。

Any changes made in the Sync Sheet Pins dialog are applied immediately, before the dialog is closed. To cancel a change made in the Sync Sheet Pins dialog, use Undo.

KiCad 自带的演示项目就是一个简单的层级结构示例video。根图纸包含七个独立的子图纸，每个子图纸都有层级标签，并且图纸引脚将根图纸中的子图纸彼此连接起来。下面显示了其中两个子图纸的符号。

An example of a simple hierarchy is the video demo project included with KiCad. The root sheet contains seven unique subsheets, each with hierarchical labels and sheet pins linking the sheets to each other in the root sheet. Two of the subsheet symbols are shown below.

该complex_hierarchy演示项目展示了一个复杂的层级结构。根图纸包含两个子图纸符号，它们都指向同一个图纸文件（ampli_ht.kicad_sch）。这使得设计可以包含同一放大器电路的两个副本。尽管这两个图纸符号指向相同的文件名，但它们的图纸名称是唯一的（ampli_ht_vertical和 ampli_ht_horizontal）。在每个子图纸中，电路除了参考标识符之外都完全相同，而参考标识符一如既往地是唯一的。

The complex_hierarchy demo project is an example of a complex hierarchy. The root sheet contains two subsheet symbols, which both refer to the same sheet file (ampli_ht.kicad_sch). This allows the design to include two copies of the same amplifier circuit. Although the two sheet symbols refer to the same filename, the sheet names are unique (ampli_ht_vertical and ampli_ht_horizontal). Inside each subsheet the circuits are identical except for the reference designators, which as always are unique.

本项目不包含任何板级引脚连接。根板与子板之间唯一的连接是使用 电源符号建立的全局电源连接。但是，如果设计需要，复杂层级结构中的板级引脚连接也可以包含在内。

This project contains no sheet pin connections. The only connections between the root sheet and the subsheets are global power connections made with power symbols. However, sheets in a complex hierarchy could include sheet pin connections if appropriate for the design.

该flat_hierarchy演示项目展示了一个扁平化的层级结构。根图包含两个独立的子图符号，没有层级引脚。本项目中的根图仅用于容纳子图，而子图也仅作为原理图中的附加页面使用。

The flat_hierarchy demo project is an example of a flat hierarchy. The root sheet contains two unique subsheet symbols with no hierarchical sheet pins. The root sheet in this project does nothing except hold the subsheets, and the subsheets are used only as additional pages in the schematic.

上面的截图中有三个错误。

There are three errors in the screenshot above.

选择 ERC 标记后，会在窗口底部的消息窗格中显示违规描述。

Selecting an ERC marker displays a description of the violation in the message pane at the bottom of the window.

有些违规情况每个网络只报告一次。例如，“输入电源引脚未被任何输出电源引脚驱动”错误实际上适用于未驱动网络上的每个输入电源引脚，但每个网络只显示一个标记。这是为了避免因单一根本原因而产生大量标记。在这种情况下，标记在原理图中的具体位置是任意的，并不一定代表解决问题的最佳位置。

Some violations are reported only once per net. For example, the "Input Power pin not driven by any Output Power pins" error technically applies to each Input Power pin on an un-driven net, but only one marker is shown per net. This is to avoid producing a large number of markers for a single root cause. In this case, exactly where the marker is placed in the schematic is arbitrary and does not necessarily indicate the ideal location for fixing the issue.

在下面的示例中，有四个未驱动的输入电源引脚（每个电源符号对应一个引脚），但只有两个 ERC 标记。添加两个PWR_FLAG符号，分别对应每个未驱动的网络，即可消除错误。符号的“正确”位置PWR_FLAG 取决于原理图，可能不在标记所在的特定电源符号附近，甚至可能不在同一张原理图上。

In the example below, there are four un-driven Input Power pins (one per power symbol), but only two ERC markers. Adding two PWR_FLAG symbols, one to each un-driven net, will clear the errors. The "correct" location for the PWR_FLAG symbol depends on the schematic and may not be near the particular power symbol where the marker was placed, or even in the same schematic sheet.

电源引脚上出现“输入电源引脚未由任何输出电源引脚驱动”错误的情况很常见，如下例所示，即使电源引脚看起来已正确连接到电源轨。这种情况通常发生在电源通过未标记为电源输出的连接器或其他组件供电的设计中。在这种情况下，ERC 检测不到任何连接到网络的输出电源引脚，并会判定输入电源引脚未由电源驱动。

It is common to have an "Input Power pin not driven by any Output Power pins" error on power pins, as shown in the example below, even though the power pins seem to be properly connected to a power rail. This happens in designs where the power is provided through connectors or other components that are not marked as power outputs. In these cases ERC won’t detect any Output Power pins connected to the net and will determine the Input Power pin is not driven by a power source.

例如，在下面的原理图中，VCC和GND连接到带有被动引脚的连接器，因此 的输入电源引脚U1不被视为由电源驱动。

For example, in the below schematic, VCC and GND are connected to a connector with passive pins, so the Input Power pins of U1 are not considered driven by a power source.

为避免此警告，请将网络连接到PWR_FLAG电源网络上的符号，如下例所示。该PWR_FLAG符号可在符号库中找到power 。或者，您可以将任意输出电源引脚连接到该网络； 该符号PWR_FLAG本身就是一个带有单个输出电源引脚的符号。

To avoid this warning, connect the net to PWR_FLAG symbol on such a power net as shown in the following example. The PWR_FLAG symbol is found in the power symbol library. Alternatively, connect any Output Power pin to the net; PWR_FLAG is simply a symbol with a single Output Power pin.

即使电源轨不需要接地，通常也需要手动添加接地网络PWR_FLAG，因为稳压器的输出被声明为“输出功率”，但其接地引脚通常被标记为“电源输入”。因此，这些稳压器不被视为驱动接地。这样做是为了防止多个稳压器共享公共接地，避免因两个“输出功率”引脚连接在一起而导致的错误。

Ground nets often need a PWR_FLAG to be manually added, even when power rails do not, because voltage regulators have outputs declared as Output Power, but their ground pins are typically marked as Power Inputs. Therefore grounds are not considered driven by these voltage regulators. This is so multiple regulators can share a common ground without errors caused by two Output Power pins being connected together.

电源网络不会“跳跃”穿过元件，因此，像无源在线滤波元件这样的元件可能需要PWR_FLAG在其下游侧进行指示，以表明该网络仍然连接到电源。

Power nets do not "jump" across components, so, components like passive inline filtering elements may need a PWR_FLAG on their downstream side to indicate that the net is still connected to a power source.

在下面的原理图中，虽然连接到连接器（和）PWR_FLAG的网络上有一个，但还需要一个来将每个和标记为电源网络，因为滤波器只有被动引脚。VCC_INGND_INPWR_FLAGVCCGNDFL1

In the below schematic, although there is a PWR_FLAG on the nets connected to the connectors (VCC_IN and GND_IN), a PWR_FLAG is also needed to mark each of VCC and GND as power nets, because the filter FL1 has only Passive pins.

VCC_IN如果“ and”网络连接到带有输出电源引脚的符号，也会出现这种情况GND_IN。实际上，在此原理图中，“and”PWR_FLAG 符号是关闭的VCC_IN，并且GND_IN是不需要的，因为这些网络上没有输入电源引脚。

This would be the case also if the VCC_IN and GND_IN nets were connected to a symbol with Output Power pins. In fact, in this schematic, the PWR_FLAG symbols are on VCC_IN and GND_IN are not required, as there are no Input Power pins on those nets.

有关电源引脚和电源标志的更多信息，请参阅 PWR_FLAG文档。

For more information about power pins and power flags, see the PWR_FLAG documentation.

原理图设置中的“违规严重性”面板允许您配置应将哪些类型的 ERC 消息报告为错误、警告或忽略。

The Violation Severity panel in Schematic Setup lets you configure what types of ERC messages should be reported as Errors, Warnings, or ignored.

原理图设置中的“引脚冲突映射”面板允许您配置连接规则，以根据相互连接的引脚类型定义错误和警告的电气条件。例如，默认情况下，当一个输出引脚连接到另一个输出引脚时会产生错误。

The Pin Conflicts Map panel in Schematic Setup allows you to configure connectivity rules to define electrical conditions for errors and warnings based on what types of pins are connected to each other. For example, by default an error is produced when an output pin is connected to another output pin.

点击矩阵中所需的方格即可更改规则，使其在以下选项之间循环切换：允许、警告、错误。

Rules can be changed by clicking on the desired square of the matrix, causing it to cycle through the choices: allowed, warning, error.

下表列出了 KiCad 检查的电气规则以及每项检查的默认违规严重程度。所有严重程度均可配置。

The table below lists the electrical rules that KiCad checks and the default violation severity for each check. All severities are configurable.

您可以使用特殊的 文本变量手动触发原理图 ERC 警告或错误。这些项目将在 ERC 运行时显示为错误或警告。这有助于标记项目以便后续跟进或审查。

You can manually trigger schematic ERC warnings or errors using special text variables. These items will appear as errors or warnings when ERC runs. This can be useful to flag items for later followup or review.

要触发 ERC 违规，请使用文本变量${ERC_ERROR <violation name>} ，${ERC_WARNING <violation name>}具体取决于您希望触发错误还是警告。您可以将其放置在文本项、文本框或字段中，包括符号字段、图纸字段和标签字段。ERC 运行时，将生成一个具有指定违规名称的 ERC 违规。这些文本变量在原理图中解析为空字符串，大括号后的任何文本都将包含在 ERC 违规描述中。文本变量必须放置在文本对象的开头才能触发违规。

To cause an ERC violation, use the text variable ${ERC_ERROR <violation name>} or ${ERC_WARNING <violation name>} depending on whether an error or warning is desired. You can place this in a text item, text box, or field, including symbol fields, sheet fields, and label fields. When ERC runs, this will generate a ERC violation with the given violation name. These text variables resolve to an empty string in the schematic, and any text after the braces is included in the ERC violation’s description. The text variable must be placed at the start of the text object in order to trigger a violation.

例如，包含以下内容的文本项${ERC_ERROR TODO}Calculate resistor value 将仅显示为文本“计算电阻值”，并且将生成一个名为“TODO”的 ERC 错误，其描述为“计算电阻值”。

For example, a text item containing ${ERC_ERROR TODO}Calculate resistor value will appear in the board as just the text "Calculate resistor value", and will generate an ERC error named "TODO" with "Calculate resistor value" in the description.

点击ERC对话框中的“保存…”按钮，即可生成并保存ERC报告文件。ERC报告文件的文件扩展名为.rpt.erc。下面提供了一个ERC报告文件示例。

An ERC report file can be generated and saved by clicking the Save…​ button in the ERC dialog. The file extension for ERC report files is .rpt. An example ERC report file is given below.

无需单独编辑每个符号的属性，可以使用符号字段表在一个位置查看和编辑设计中所有符号的属性。这包括通过编辑 Footprint每个符号的字段来分配封装。

Rather than editing the properties of each symbol individually, the Symbol Fields Table can be used to view and edit the properties of all symbols in the design in one place. This includes assigning footprints by editing the Footprint field of each symbol.

可以通过“工具” → “编辑符号字段…”或通过 顶部工具栏上的按钮访问符号字段表。

The Symbol Fields Table is accessed with Tools → Edit Symbol Fields…​, or with the button on the top toolbar.

该Footprint字段在此处的行为与“符号属性”窗口中的行为相同：可以直接编辑，也可以使用封装库浏览器以可视方式选择封装。

The Footprint field behaves the same here as in the Symbol Properties window: it can be edited directly, or footprints can be selected visually with the Footprint Library Browser.

有关符号字段表的更多信息，请参阅 有关编辑符号属性的部分。

For more information on the Symbol Fields Table, see the section on editing symbol properties.

下图显示了足迹分配工具的主窗口。

The image below shows the main window of the Footprint Assignment Tool.

顶部工具栏包含以下命令：

The top toolbar contains the following commands:

下表列出了“封装分配工具”的键盘命令：

The following table lists the keyboard commands for the Footprint Assignment Tool:

要手动将封装与元件关联，首先在元件（中间）窗格中选择一个元件。然后，在封装（右侧）窗格中双击所需封装的名称来选择封装。封装将被分配给所选元件，并且下一个尚未分配封装的元件将自动被选中。

To manually associate a footprint with a component, first select a component in the component (middle) pane. Then select a footprint in the footprint (right) pane by double-clicking on the name of the desired footprint. The footprint will be assigned to the selected component, and the next component without an assigned footprint is automatically selected.

当所有元件都分配好封装后，单击“确定”按钮保存分配并退出工具。或者，单击“取消”放弃更新后的分配，或单击“应用”、“保存原理图并继续”以保存新的分配而不退出工具。

When all components have footprints assigned to them, click the OK button to save the assignments and exit the tool. Alternatively, click Cancel to discard the updated assignments, or Apply, Save Schematic & Continue to save the new assignments without exiting the tool.

封装分配工具允许您将封装分配存储在外部文件中，并在以后加载这些分配，即使是在不同的项目中。这样，您可以自动将符号与相应的封装关联起来。

The Footprint Assignment Tool allows you to store footprint assignments in an external file and load the assignments later, even in a different project. This allows you to automatically associate symbols with the appropriate footprints.

外部文件称为等效文件，它存储了符号值到相应封装的映射关系。等效文件通常使用.equivalence.equ文件扩展名。等效文件是语法简单的纯文本文件，必须由用户使用文本编辑器创建。语法说明如下。

The external file is referred to as an equivalence file, and it stores a mapping of a symbol value to a corresponding footprint. Equivalence files typically use the .equ file extension. Equivalence files are plain text files with a simple syntax, and must be created by the user using a text editor. The syntax is described below.

您可以通过在“封装分配工具”中单击“首选项” → “管理封装关联文件”来选择要使用的等效文件。

You can select which equivalence files to use by clicking Preferences → Manage Footprint Association Files in the Footprint Assignment Tool.

窗口底部会显示相关的环境变量。 选中“相对路径”选项后，这些环境变量将自动用于创建相对于项目或封装库的所选等效文件路径。

Relevant environment variables are shown at the bottom of the window. When the Relative path option is checked, these environment variables will automatically be used to make paths to selected equivalence files relative to the project or footprint libraries.

将所需的等效文件按正确的顺序加载后，单击 封装分配工具顶部工具栏中的按钮即可执行自动封装关联。

Once the desired equivalence files have been loaded in the correct order, automatic footprint association can be performed by clicking the button in the top toolbar of the Footprint Assignment Tool.

所有在已加载的等效文件中具有值的符号都会自动分配封装。但是，已经分配了封装的符号将不会更新。

All symbols with a value found in a loaded equivalence file will have their footprints automatically assigned. However, symbols that already have footprints assigned will not be updated.

封装分配工具包含一个封装查看器。单击 顶部工具栏中的按钮即可启动封装查看器并显示所选封装。

The Footprint Assignment Tool contains a footprint viewer. Clicking the button in the top toolbar launches the footprint viewer and shows the selected footprint.

顶部工具栏包含以下命令：

The top toolbar contains the following commands:

左侧工具栏包含以下命令：

The left toolbar contains the following commands:

该工具提供了多种控制其行为的选项。

The tool has several options to control its behavior.

符号和封装通过唯一标识符（也称为 UUID）关联起来。这些标识符在 KiCad 中自动处理，通常对用户不可见。即使参考标识符发生更改，它们也能确保符号及其对应的封装在原理图和 PCB 之间保持关联。新对象在创建时会被分配标识符。

Symbols and footprints are linked together using unique identifiers (also called UUIDs). These are handled automatically within KiCad and are not usually visible to users. They allow a symbol and its partner footprint to keep their connection between schematic and PCB, even if the reference designator is changed. New objects get assigned their identifiers upon creation.

该工具提供了多种控制其行为的选项。

The tool has several options to control its behavior.

也可以通过从 PCB 编辑器导出 CMP 文件（文件→导出→封装关联 (.cmp) 文件… ​）并将其导入原理图编辑器（文件 →导入→封装分配… ​）将选定的更改同步回原理图。

Select changes can also be synced from the PCB back to the schematic by exporting a CMP file from the PCB editor (File → Export → Footprint Association (.cmp) File…​) and importing it in the Schematic Editor (File → Import → Footprint Assignments…​).

绘制的 PDF 文件可以选择性地包含多个交互式功能。

Plotted PDFs can optionally have several interactive features.